Ebook Advanced catia v5 workbook

ADVANCED
CATIA V5 Workbook
Knowledgeware and Work Benches





















Richard Cozzens
Southern Utah University
www.suu.edu/cadcam

SDC

Schroff Development Corporation

www.schroff.com

www.schroff-europe.com

PUBLICATIONS
Releases 12 & 13
Tutorial Exercises
Knowledgeware
Work Benches
Kinematics
Stress Analysis
Sheetmetal Design
Prismatic Machining
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Figure 1.1
Lesson 1 K
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Introduction to CATIA V5 Knowledgeware

Knowledgeware is not one specific CATIA V5 work bench but several work benches.
Some of the tools can be accessed in the Standard tool bar in the Part Design work
bench. Simply put, Knowledgeware is a group of tools that allow you to create,
manipulate and check your CATIA V5 creations.





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Lesson 1 Objectives

This lesson will take you through the process of automating the creation of joggled
extrusions as shown in Figure 1.1. At the end of the lesson you should be able to do the
following:

1. Create the Extrusion Profile Sketch and Joggle Profile Sketch.
2. Assign variable names to the required constraints.
3. Create the Joggled Extrusion.CATPart using the Rib tool.
4. Create a spreadsheet with aluminum extrusion dimensions.
5. Link the spreadsheet to the Joggled Extrusion.CATPart.
6. Apply the spreadsheet to update the Joggled Extrusion.CATPart.
7. Create a Macro.
8. Modify the Macro using VB Script.
9. Create prompt windows for input using VB Script.
10. Check for company/industry standards using the Check tool.
11. Implement the updated Joggled Extrusion.CATPart in a dimensioned drawing.

Figures 1.1 and 1.2 show examples of the Joggled Extrusion you will create in this
lesson. Figure 1.1 shows the standard Joggled Extrusion along with its Specification
Tree. Figure 1.2 shows a spreadsheet with the resultant dimensioned drawing.
Figure 1.2
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Knowledgeware Work Bench Tools and Tool Bars

A combination of six tool bars is used in this lesson from the Knowledgware Product.
The Knowledgeware Product is made up of the following work benches; Knowledge
Advisor, Knowledge Expert, Product Engineering Optimizer, Product Knowledge
Template, Product Function Optimization and Product Functional Definition. Each
of these work benches has a different combination of tools in each tool bar. If you switch
between any of these work benches you may see the same tool in a different tool bar. For
example the Formula and Design Table tools are accessible from many workbenches in
the bottom tool bar.

The Set of Equations Tool Bar
This tool bar contains only one tool.
TOOL ICON TOOL NAME TOOL DEFINITION

Set Of Equations
Solves a set of equations.


The Knowledge Tool Bar




TOOL
ICON
TOOL NAME TOOL DEFINITION

Formula
Creates parameters and determines the
relationship between parameters.

Comment &
URLs
Adds URLs to the user parameters.

Check Analysis
Toolbox
Signals when there has been a violation in a
check and/or rule.

Design Table
Creates and/or imports design tables
(spreadsheets).

Knowledge
Inspector
Queries a design to determine and preview the
results of new parameters.


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The Reactive Features Tool Bar

TOOL ICON TOOL NAME TOOL DEFINITION

Select
Highlights the element you want to select.

Rule
Creates a rule and applies it to your document.

Check
Creates a check and applies it to your document.

Reactions
Creates a script that will change feature attributes.


The Tools Tool Bar




TOOL ICON TOOL NAME TOOL DEFINITION

Measure
Update
Updates relationships.

Update

Updates the CATPart and/or CATProduct.


The Actions Tool Bar




TOOL ICON TOOL NAME TOOL DEFINITION

Macro with
Arguments
Opens a macro with arguments.

Actions
Creates a script.

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The Organize Knowledge Tool Bar




TOOL ICON TOOL NAME TOOL DEFINITION

Add Set of
Parameters
Creates a set of parameters.

Add Set of
Relations
Creates a set of relations.

Parameters
Explorer
Adds new parameters to a feature.

Comment &
URLs
Adds URLs to the user parameters.


The Control Features Tool Bar

TOOL ICON TOOL NAME TOOL DEFINITION

List
Manage the objects you want to add to the list
you are creating.

Loop
Interactively apply a loop to an existing
document.












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The Problem:

One of the many Metalcraft Technologies Inc. (MTI) fabrication processes is fabricating
a joggle in standard and non-standard extrusions. Most of the extrusion requirements are
contained in large assembly mylar sheets. Most of the drawings (mylars) were created in
the early 1970s. It is difficult for the engineer/planner to read and/or measure the mylar
accurately. It may take the engineer/planner 10 to 30 minutes to verify he/she has found
and applied the correct dimensions. It is not productive for the fabricator to also have to
go through the same time consuming process. Having the drawing interpreted so many
times by so many different people will inevitably introduce more chances for error. It is
MTI’s policy that the engineer/planner creates an individual drawing for each joggled
extrusion to avoid such confusion. MTI has minimized the time required to create the
individual drawings by setting up templates and standards. Yet, even with templates and
standards this process is still time consuming. Each drawing is basically the same but has
to be re-created because of a few simple dimensional differences and/or a different type

of extrusion. The goal was to cut this time down by using the intelligence contained in
the existing standard extrusion.



The Solution:

CATIA V5 Knowledgeware tools allow the user to capture and use the intelligence
contained within the standard Joggled Extrusion.CATPart. CATIA V5 macro and
scripting capabilities allow the user to be prompted for the critical dimensions. CATIA
V5 then takes the information and updates the Joggled Extrusion.CATPart according to
the supplied input. CATIA V5 also automatically updates the standard dimensioned
drawing (CATDrawing). The dimensioned drawing is ready to be released to the
production floor in a matter of minutes instead of 30 to 60 minutes.

An additional advantage to this process is adding dimensional checks. If the dimensional
values do not match the company and /or industry standards the user will get a warning.

The following instructions will take you through the steps of creating the standard
Joggled Extrusion.CATPart and then implementing the Knowledgeware solution
described above.






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Steps to Implementing the Knowledgeware Solution

A parameterized sketch/solid is a basic form of Knowledgeware; it contains intelligence.
Prior to parametric applications you would have to create each variation of the extrusion
from scratch. Parametric applications allow you to modify one constraint and the
extrusion (solid) will update to that constraint.


1. Determine the Requirements

The general problem solving skills apply to implementing the Knowledgeware
solution. You need to list all that is known and unknown and you need to list all of
the variables, for example, what is known.

If you are not sure at first, manually go through the process. You must be able to
create the process manually.

2. Creating the Extrusion Profile Sketch

Create an Extrusion Profile sketch on the ZX Plane as shown in Figure 1.3. The 0,0
point is located at the lower left corner of the extrusion. This sketch will be used as
the standard; all other extrusions will be derived from this basic sketch. When you
complete the sketch, exit the Sketcher work bench but do not use the Pad tool to
create a solid. The solid will be created in Step 8 using a different tool.

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Figure 1.3




3. Constraining the Extrusion Profile Sketch

After completing the rough sketch of the Extrusion Profile sketch as shown in
Figure 1.3 you must constrain it similar to the constrains shown in Figure 1.3.

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4. Modifying the Constraint Names

In this particular step it is critical that you rename the constraints. Understand that it
is not absolutely necessary, but it will make this process a lot easier if you rename the
constraints with a name that signifies what it is constraining. If you have problems
remembering what the constraint name is, write it down; the names will be required
to create the spreadsheet later in this lesson. It is suggested that you use the
constraint names shown in Figure 1.4 so your information matches what you will see
throughout the remaining steps into this lesson. Also, change the branch name
Sketch.1 to Extrusion Profile. Once you have successfully completed this lesson it is
suggested that you try different variations of this process.

Circle Constraint = R5
Offset Constraint = T2
Figure 1.4
Circle Constraint = R1
Offset Constraint = B
Offset Constraint = T1
Circle Constraint = R2
Circle Constraint = R
Circle Constraint = R3 Offset Constraint = A
Circle Constraint = R4
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Figure 1.5
Constraint by selecting on line (length)
Constraint between two entities (distance)
Constraint by selecting the radius
Constraint between two entities (distance)
Figure 1.3 shows the constraints in the Specification Tree already renamed. CATIA
V5 will automatically give it a name as shown in Figure 1.5 below.

Complete the following steps to rename the constraints.

4.1 Double click on the constraint that you want to rename. This will bring up
the Constraint Definition window with the constraint value in it.

4.2 Select the More button. This will bring up a Constraint Definition
window as shown in Figure 1.6.

4.3 Edit the current constraint name in the Name box to what you want the new
constraint to be named.

4.4 Select OK. The newly renamed constraint will show up in the
Specification Tree.






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5. Creating the Profile Sketch of the Joggle

This step, like Step 2, requires you to create another sketch. This sketch
is created on the YZ Plane in the negative direction (notice where the
is located in relation to the sketch in Figure 1.7). Use the information in
Figure 1.7 to create the Joggle Profile sketch.



Figure 1.6
Figure 1.7
Offset Constraint =
Depth
Offset Constraint =

Transition
Distance Constraint (length) = Dist. To
Endp.
Distance Constraint (length) =
Length.50
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6. Constraining the Joggle Profile Sketch

Create constraints for the Joggle Profile sketch similar to the ones shown in
Figure 1.7.

7. Modifying the Constraint Names

Modify the constraint names you created in Step 6 to match the constraint names
shown in Figure 1.7. Step 4 describes the process of renaming constraints.

NOTE: It is important that the constraint names be consistent throughout this lesson.
The names will be used to link the information to a table in the next few
steps. If you deviate from the naming convention used in this lesson, the
remaining steps will not work as described.


8. Creating a Solid of the Joggled Extrusion

Now that both sketches are created you are ready to create the solid. This will be
accomplished by using the Rib tool found in the Part Design work bench. Complete
the following steps to create the solid

8.1 Select the Extrusion Profile sketch created in Step 2. Make sure it is
highlighted.

8.2 Select the Rib tool found in the Part Design work bench. This will bring up
the Rib Definition window as shown in Figure 1.8. The prompt zone will
prompt you to Define the center curve. The Extrusion Profile will be
listed in the Profile box.

8.3 The Center Curve box should be highlighted. Select the Joggle Profile
either from the geometry or the Specification Tree. CATIA V5 will give
you a preview of the Extrusion Profile being extruded along lines that

define the Joggle Profile sketch.












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8.4 If the preview looks similar to the joggled extrusion that is shown in Figure
1.9, select the OK button to complete the operation. The Joggled
Extrusion will be made into a solid.


Now that you have created a solid “Joggled Extrusion,” you are ready to go on to the
next step: creating a table of different types of extrusions.













Figure 1.8
Extrusion Profile Sketch
Joggle Profile Sketch
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9. Creating an Extrusion Table


Figure 1.10 is an Excel (Spreadsheet) that contains the dimensions to four different
types of aluminum extrusions. The extrusions and their dimensions were taken from
the Tierany Metals Catalog. You might recognize the extrusion on row 5; it is the
one you created in the previous steps. If you wanted to create the extrusion in row 2
you would have to start from step one again or you could go back to the Extrusion
Profile sketch and revise the constraints. Obviously revising the constraints would be
the quickest and easiest method to creating the new extrusion. CATIA V5
Knowledgeware tools can make this process even quicker and easier. This is

accomplished by linking the Excel File to the CATPart.
Figure 1.9
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You can use an existing spreadsheet if it is available. If it is not available, you will
have to create your own. The spreadsheet does not have to be an Excel program; any
spreadsheet program will work. Each column requires a header. The header will be
used as a variable link later in the lesson. Notice the column headers used in Figure
1.10 match the constraint names used in the previous steps to create the Extrusion
Profile sketch. This is not absolutely necessary, but it does make the linking process
much more intuitive.

To complete this step, go into the spreadsheet program of your choice and enter the

information in as shown in Figure 1.10. Save the file; preferably in the same
directory that your CATPart file exists. Remember the file name and where it exists
as you will need that information in the following step.


10. Importing the Extrusion Table

CATIA V5 allows you to create a design table inside CATIA V5 or import an
existing design table. This step will show you how to import the design table created
in Step 9. As you go through the process of importing a design table, you will be
able to observe how CATIA V5 allows you the opportunity to create and modify a
design table inside of CATIA V5. To import a design table, complete the following
steps.

10.1 In the Part Design work bench, double click on the Design
Table tool. The Design Table tool is located in the
Standard tool bar at the bottom of the CATIA V5 screen.
The Design Table tool icon is shown in Figure 1.11. This
will bring up the Creation of a Design Table window as
shown in Figure 1.12.

10.2 Name the design table “Extrusion Table” using the Name box as shown in
Figure 1.12.

Figure 1.11
Figure 1.10
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Figure 1.12



10.3 The Comment box will automatically place the date of creation. You can
modify this box to any text that might help. This is just a comment box and
will not have any effect on the following steps.

10.4 Select Create a design table from a pre-existing file. Although you will
not use the other choice in this lesson it is important that you know that the
other choice is available. The other choice is Create a design table with
current parameter values. This choice allows you to create a design table
inside CATIA V5.

10.5 Select the OK button. This will bring up browser window labeled File
Selection. This is the standard Windows file browser. Reference Figure
1.13.

10.6 Select the directory and the file that you want to import. For this step, you
will want to select the Extrusion Table created in Step 9, as shown in
Figure 1.13.

10.7 Select the Open button. This will bring up an Automatic Associations?
window as shown in Figure 1.13. The prompt window asks if you want to
automatically associate the parameters.

10.8 Select Yes. This will bring up the Extrusion Table Active window as
shown in Figure 1.14. Note that Figure 1.14 is shown with the
Associations tab selected, not the Configurations tab. If there are no
associations listed in the Configurations box, CATIA V5 was not able to
automatically associate any of the Constraint Parameters or Extrusion
Table Column Headings.

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Figure 1.13

10.9 When CATIA V5 is not able to automatically associate the two together,
you will have to manually associate them. To do this, select the
Associations tab in the Extrusion Table Active window as shown in
Figure 1.14.

10.10 The Parameters box lists all the parameters CATIA V5 created in the
Extrusion Profile sketch. A CATIA V5 sketch contains a lot of
parameters that the users are not usually aware of. What makes it more
difficult, is the CATIA V5 naming convention. It is difficult to identify a
CATIA V5 parameter listed in this box to an actual parameter in the
Extrusion Profile sketch. This is where renaming the constraints in the
previous steps will prove to be beneficial. You should be able to scroll
through the Parameters box and identify the constraints you renamed.
All the parameters are represented on two separate lines. For this lesson
you will use the line that ends with a type of measurement such as Radius,
Offset or Length. You will not use the line ending in Activity. For this
step, scroll through the Parameters list; verify the constraints you
renamed in Step 4 are listed.




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10.11 Select A from the Columns box.

10.12 From the Parameters box, find and select the line ‘PartBody\Extrusion
Profile\A\Length’.

10.13 Select the Associate button. Your two selections from the Parameters
and Columns boxes will show up in the Associations between
parameters and columns box. This means that they were successfully
associated.

10.14 Continue this process until all the variables in the Columns box, except
for Extrusion Number, is matched up to the appropriate parameter. (R,
R1, etc. will of course be a Radius rather than a Length).

Figure 1.14

Box as it appears
after selecting all
parameters.
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Figure 1.15
10.15 Now you can take care of the Extrusion Number column heading. The
Extrusion Profile sketch has no associative value to the Extrusion
Number that was created in the Extrusion Table. You can assign it one
by selecting the Extrusion Number in the Columns box.

10.16 Select the Create Parameters… button. This will bring up the OK
Creates Parameters for Selected Lines window as shown in Figure 1.15.

10.17 Make sure Extrusion Number is selected/highlighted.

10.18 Select the OK button. This will create an association of a string type to
the Extrusion Number heading. The association will be displayed in the
Extrusion Table Active window under the Associations tab along with
all the other associations you created in this step. What this really does for
you is allows the Specification Tree to show the Extrusion Number.
Figure 1.16, under the Parameters branch, displays ‘Extrusion Number’
=60-10677. The string of numbers 60-10677 is linked from the specific
row in the Extrusion Table. If you select another row (extrusion) from
the Extrusion Table the Specification Tree will reflect the change just as
the solid does.

NOTE: In order for the parameters to show up in the Specification Tree you must
have the Options set correctly. Step 13 will show you how to set the
correct options.

10.19 Select the Configurations tab in the Extrusion Table Active window. If
you correctly associated the Parameters and Columns, it should look
similar to the table shown in Figure 1.16. If your window looks similar to
the one shown in Figure 1.16, select the OK button to complete the
association process.

10.20 Doing this will make the window disappear and Extrusion Table.1 shows
up on your Relations branch of the Specification Tree. You may wonder
what else is different. What did you just accomplish? Step 11 will show
you the advantages of what you just accomplished.
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11. Applying the Extrusion Table to the Joggled Extrusion

The purpose for linking a design table to the CATPart file is to update the part
without having to redraw and/or revise the constraints manually. (Keep in mind that
if you move your saved table, it will break the link and you will need to re-link it.)
To test this, complete the following steps.

11.1 Double click on Extrusion Table in the Specification Tree. This will
bring up the Extrusion Table Active window as shown in Figure 1.16.
The data in row 1 is currently the active row. There are several methods to

tell which row of data is active.

Figure 1.16
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Figure 1.17
11.1.1 The window label contains the information: Extrusion Table
active, configuration row: 1.

11.1.2 Row 1 has brackets around it [<1>]. The inactive lines do not
have the brackets around it.

11.1.3 One other method is to check the data against actual extrusion
dimensions. Figure 1.16 and the entire product in the previous
steps represent the data that is contained in row 1.

11.2 To make row 4 (Extrusion Number 60-13028) active, select the row. The
existing extrusion will turn red signifying it needs to be updated.

11.3 Select the OK button. This will update your active extrusion to the data
contained in row 4. Figure 1.17 shows the row 4 extrusion. Compare the
differences between the extrusion represented in Figure 1.16 and 1.17.
Verify the extrusions with the dimensions in the Extrusion Table (design
table).

NOTE: If your extrusion does not automatically update you will have to select the
Update button in the Standard tool bar section to force the solid to update.
If you want CATIA V5 to automatically update select T
ools, Options,
Infrastructure branch, Part Infrastructure branch, General tab, Update
section and select the Automatic button.

Once you link your Extrusion Table to your CATPart, updating is quite simple.
Click on the Extrusion Table in the Specification Tree to bring up the design table.
Select the row of data you want to apply to the CATPart and select OK. Be sure to
select row 1 (Extrusion Number 60-10677) again before moving on to the next step.








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12. Editing the Extrusion Table

You now have the Extrusion Table linked to the Joggled Extrusion CATPart. As
the previous step demonstrated, creating new extrusions are only a few clicks away.
Editing the Extrusion Table (design table) is just as easy. Modifying the Extrusion
Table can be done in CATIA V5 or outside of CATIA V5. To modify the
Extrusion Table inside of CATIA V5, complete the following steps.

12.1 Double click on the Extrusion Table in the Specification Tree.

12.2 This brings up the Extrusion Table Active window. Click on the Edit
Table button at the bottom left of the window.

12.3 This brings up the original spreadsheet that the Extrusion Table was
created in. Modify the number 2 in row 2 (Extrusion Number 60-10677)
and column C (header B (in)) to a 4.

12.4 Save and exit the revised spread sheet program. CATIA V5 will notify you
that the Extrusion Table has been revised. Select Close to update the link.

12.5 The part will turn red because it is the active row. Select OK to update the
Joggled Extrusion CATPart.

Your part is now updated to the information edited into the spreadsheet without
leaving CATIA V5. You can use this method to add rows of new information, in
this case additional extrusion types. You can also delete rows of information. The
second method of revising the spreadsheet is editing the spreadsheet outside of
CATIA V5. CATIA V5 will still give you a warning and a chance to accept or reject
the revised spreadsheet.

NOTE: 2″ is correct for the 60-10677 Extrusion Number, so be sure to change it
back.


13. Displaying the Extrusion Type in the Specification Tree

Figure 1.18 shows the Specification Tree without the value displayed, and Figure
1.19 shows the Specification Tree after the following process to display the value.
Select T
ools, Options, Parameters and Measure under the General branch,

Knowledge tab, Parameters Tree View section; check the With Value box.








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14. Modifying the Existing Joggle Profile Sketch

The previous steps showed you how to create, select and automate the creation of
different types of extrusions. This was accomplished using a spreadsheet and the

Extrusion Profile sketch. The following step will show you how to apply joggle
information to the selected extrusion. This step uses/modifies the Joggle Profile
sketch. If joggle information was standardized, you could create a spreadsheet with
the required information and apply it to the Joggle Profile sketch as you did to the
Extrusion Profile sketch. Joggle information is not standard; it is as varied as the
parts and assemblies they are applied to. With the help of Knowledgeware this
process can still be automated by getting information directly from the user in the
place of the spreadsheet.

For this step, revise all the constraints in the Joggle Profile sketch to match the
constraints shown in Figure 1.16.

Figure 1.18
Figure 1.19
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Figure 1.20
The following steps will show you how this is accomplished. This step will start out
real basic so you can better appreciate the power of CATIA V5’s Knowledgeware.
The Joggle Profile sketch controls the joggle of the extrusion. If you want to
change the joggle depth, you could go into the Joggle Profile sketch and revise the
constraint that controls the depth. Figure 1.7 shows that value of Depth is currently
.75″. Entering the Joggle Profile sketch and modifying all the constraints for every
individual part becomes very repetitious and time consuming. The following steps
will show you how Knowledgeware can help you automate this process.


15. Automating the Modification Using a Marco

This step is similar to what was explained in Step 12. You go through the same
steps except that you turn on the Macro Recorder to record everything you do. To
accomplish this, complete the following steps.

15.1 Enter the Joggle Profile sketch, as shown in Figure 1.7. The first thing you
need to remember is to record only what is necessary, other wise you get a
lot of information that only complicates the process.



15.2 Select Tools, Macro, Start Recording. This will bring up the Record
Macro window as shown in Figure 1.20.

15.3 The Current Macro Library Or Document: should default to your
CATPart at its designated saved location. Select CATScript for the
Language Used: box.


15.4 Name the macro “JoggleDimensions.CATScript.” CATIA V5 will
default the name to Macro1.catvbs unless you specify a name. You must
also add the .CATScript extension. Adding the extension allows CATIA
V5 to save the macro externally not only as a macro but also a CATScript.